Abstract. Introduction:

Transcription

1 Abstract This project analyzed a lifecycle test fixture for stress under generic test loading. The maximum stress is expected to occur near the shrink fit pin on the lever arm. The model was constructed using 3D solid quadratic elements without reduced integration. Interaction properties and boundary conditions were defined between the pin, lever, and drive shaft. The resolved loads were then applied to the lever arm. The model was partitioned and then meshed using structured meshes. The program could not correctly run using the press-fit definitions. Only one of the press-fits would be active at a time, leading to model modifications. These modifications included removing the pin, adding tie constraints between the drive shaft and lever am, and adding more boundary conditions at the pin location. Results obtained from this model were within magnitude of the hand calculations. The von Mises stress of the lever arm was approximately 1062 psi, while the hand calculations yielded a value of 1685 psi. The overall vertical deflection of the system was.0027 inches, which is realistic for the scale of the project Introduction: The system that will be analyzed is a life-cycle validation test fixture that was designed for testing at Alcon Laboratories Incorporated. This test fixture was created in order to test the monitor hinges for fatigue and wear over the lifetime of the product. The test included rotating the monitor from +25 o to 180 o (referencing the vertical axis) 7,530 times per monitor during testing. Wear would then be noted once testing was completed. A servomotor, geared down 50:1, drove the lever arm during testing and controlled using PLC s. The servomotor was more powerful than necessary for this application, thus will be able to provide sufficient torque to operate the system for all ranges of motion. The key in this test was maintaining the correct angle of rotation in order to correctly test the displays, and avoid damage. Figure 1 shows a solid model with skeleton of the component to be tested and the system. The final testing unit is depicted in Figure 2, without the display. Figure 1. Fixture solid model with skeleton. Figure 2. Final production lifecycle test fixture. Desired Outcomes: The critical portion of this system is the lever arm that is used to rotate the monitor. The drive shaft is sent through a bearing, which provides x-y stability but allows free rotation of the shaft. This shaft is then fit into the lever arm itself with a press fit pin inserted between the two, to ensure that the rotation is exact between the drive shaft and lever arm. This lever arm - 1 -

2 extends and holds the monitor support, which is of a glove type design in order to avoid damage to the monitor. The lever arm experiences a number of forces during monitor rotation. It sees the moment being applied at the end due to the monitor resisting rotation as well as the weight of the monitor glove. The drive shaft transfers a torque equal to or greater than the weight of the unit in order to rotate. This resistance to rotation and weight also create torques within the lever arm since it is offset. In addition to this, the lever arm possesses press fit cylinders on both sides. These features ensure that the lever arm and servo maintain the same angle during program cycling. Solid model close-ups of the lever arm are shown in Figures 3-4. Figure 3. Lever arm with glove. Figure 4. Lever arm. The highest stresses in the arm will occur where the drive shaft is press fit. It sees the highest stress due to bending, torque, and press fit at this point. Deflection is only a minor issue in this analysis since it is constrained by the press-fit cylinder. There will be some bending deflection at the end, but the stress is the main concern. The material used for this part is anodized 6061-T6 Aluminum. The stresses in this analysis will not cause yielding in the part, but I will investigate the lifetime of the component. Since it is used for lifecycle validation, the lever arm will see a large number of cycles. It is also adaptable to other size screens and newer product lines, which further enhance the amount of use it will see. The goal is to use the FEA data to find the maximum stresses that the aluminum lever arm will be experiencing during testing, to ensure that it has been sufficiently designed. Proposed Analysis: Hand calculations of press-fit forces, torques due to monitor forces, and bending due to monitor forces will need to be done at the location of the drive shaft. The glove lever attachment needs to have a preliminary analysis done to see if a fixed assumption is valid. It is connected through two cylinders passing through the lever, screwed into the glove. The torque due to the glove will need to be investigated at this point in order to see if a stress concentration exists within the cylinders. After this data is obtained, the method of modeling within ABAQUS can be determined. The data will show if the connectors at the glove can be ignored, since they are a large distance from the area seeing the highest stress. If they turn out to be a center of interest, then they will need to be modeled in detail. The actual model itself does not need to contain the glove unit since the forces can be applied directly to the lever arm itself, once translated. The drive shaft is contained within a bearing, which can be considered fixed in the x-y directions. The bearing will act as a boundary condition that prevents all rotation and translation. The model will be analyzed both with and without the press-fit pin in order to see the effect on the overall stresses

3 Approximate Solution: Hand calculations were completed in order to have an idea of the system stresses. An estimation of the press-fit for both the 6061-T6 aluminum lever arm and 303 CRES stainless steel drive shaft was calculated using the compound pressure vessel equations. This is an estimation since the parts are not completely circular in the radial direction. Hand calculations estimating the stress in the lever arm due to the force of the glove were then completed. Estimates of the stress concentration factor had to be made since there were holes along 2 axes within the arm. A force of roughly 6.34 lb is applied on the glove, which yields a torque of 31.7 lb applied on the lever arm. See Figure 5 for a schematic of the loading, Table 1 for results of the hand calculations, and Appendix A for the preliminary hand calculations lb F = 6.34 lb T = 31.7 lb-in Figure 5. Left: Actual loading schematic. Right: Load resolution onto lever arm. Table 1. Summary of hand calculations. All stresses are in [psi], with the Von Mises Stress being calculated using only the moment and torque stresses. Lever Arm Drive Shaft σ r σ θ τ max σ moment σ e σ r σ θ Model development: All of the parts were initially created using SolidWorks, and converted to IGS files. The IGS files were then imported into ABAQUS for analysis as 3-D solids, with precise geometry. By doing roecise geometry, it minimized the amount of geometry repair that would need to be done. There was not much defeaturing that needed to be done, other than the point of load application. On the actual lever arm, there are two screws that hold the lever to the glove. This is the point where the loads are applied. For simplification, these holes were left out, an the loads were applied at a point, where the glove would attach. This eliminated two holes and made the meshing much easier. Additionally, this deafeaturing occurred far enough away from the point of interest that it would not significantly effect the results. When the parts were imported, a geometry cleanup needed to be done in order to smooth out some of the edges. Using the Figure 6. Boundary condition Geometry Repair Merge Edges tool, the edges were combined zone and partitions. into one smooth edge. The proper material definitions of 6061 T6 aluminum and 303 CRES stainless steel were then applied to the appropriate parts

4 The model needed to be a 3-D solid in order to model the stresses due to the press-fit pin. Initially, a model of the pin, lever arm, and drive shaft assembly was created. A single boundary condition of no rotation or translation was applied on the drive shaft where it was inserted into the bearing. A partition needed to be created on the part in order to do this (Figure 6). I found that manipulating the geometry, inserting datums, and partitions was much more difficult since the parts had been created outside of ABAQUS. Once the boundary condition was applied, the resolved loads were applied onto the lever arm. Initially, I applied a downward force, and a torque at the point of action. Once again, a partition and datum needed to be created in order to do this. Two interactions were then created between the press fit pin and the lever arm / drive shaft. These interactions needed to represent the press-fit condition of the pin. To do this, a surfaceto-surface contact interaction was created. The lever arm and drive shaft acted as the master surfaces, while the pin acted as the slave surface. According to the manual, automatic overclosure could only be resolved during the first step, so both interactions were placed in the first step of the analysis. The contact property defined for both of the press-fits were simply normal behavior with hard contact. This was per the specifications of the ABAQUS users manual. The loads were then placed in their own step, after the overclosure resolution, so that ABAQUS would solve the press-fits, then apply the necessary loads. Boundary conditions were held during all of the steps. Overall, developing the initial model was relatively simple. The only issues that occurred were due to the inaccessibility of the parts, since they were imported from SolidWorks. More issues occurred once the assembly was submitted for analysis. These problems are detailed in the Analysis section. The problems resulted in having to create a second model without the press fit pin. Instead of the press-fit pin, a boundary condition of no rotation or translation was created on the inside faces of the lever and drive shaft. The holes were not removed using defeaturing because of the interest in the stress concentration. Other than this, the model remained the same. Mesh development: As stated, this model uses 3-D solid elements. Initially, ABAQUS would not generate a mesh of the parts using anything but bottom-up. I attempted to use the bottom-up mesh tool, but it would not create a sufficient mesh. An alternative to using the bottom-up mesh is to partition the 3-D model into smaller sections. Apparently, ABAQUS can create structured and other types of meshes, if the model is split up into smaller pieces. The complex geometry of the fixed end of the lever can be broken up in this way, in order to achieve meshing. Figure 6 shows the partitions created for the fixed end of the shaft. Partitions were not needed at the other end of the lever arm due to the simple geometry. Once partitioned, a structured, hex-dominated mesh was created on all parts. I initially used just a hex mesh, but ABAQUS stated there would be no difference between hex and hex-dominated, so hex-dominated was used for all meshes. By partitioning, this allowed for different mesh sizes depending on the interest in that portion of the model. As can be seen in Figure 7, the mesh size varied Figure 7. Mesh setup - 4 -

5 depending on location. The area of interest around the hole possessed the smallest element size, with the larger element sizes appearing further from the hole. The partitions that were created proved to be useful when creating the varying mesh size. To change the mesh size, I used the Seed Edge By Size tool. Initially, a linear element type was used. When a convergence study was performed, the model did not converge to a value prior to the computer running out of committed memory. The amount of elements ballooned to a level that required too much computation power and time. A mesh convergence plot with realistic amounts of elements was achieved using quadratic elements (no reduced integration). Once the type of element was determined, the parts were meshed. The final data for the converged mesh can be found in Table 2. This data is for the model with no pin, since that would prove to be the final model used for calculations. Table 2. Summary of mesh data. Part # Elements # DOF Aspect Ratio > 5 Face Corner Angle > 135 Warning % Face Corner Angle < 45 Overall Analysis Warnings Lever Arm Drive Shaft The overall warnings encountered were for less than 5% of the overall elements, which means that it is sufficient for this type of analysis. The system is not operating near failure, so it is not critical that all elements be of extremely high quality. Analysis: For this model, a static stress analysis is sufficient. The model experiences relatively small deflections, so linear material analysis can be used. Below are listed all of the errors and warnings that were obtained during the analysis. Error 1 nodes have inactive dof on which boundary conditions are specified. Too many attempts made for this increment STANDARD_MEMORY IS CURRENTLY SET TO MBYTES, BUT MORE MEMORY IS REQUIRED. Interpretation, Solution A moment cannot be applied to a node of a 3D solid. The node does not have rotational degrees of freedom. In order to fix this, I reduced the torque on the lever arm to a force couple, which eliminated the error. This error meant that a solution could not be reached within the given amount of increments per step. I adjusted the number of increments from 100 to 4 to try and fix this error, but it persisted. This error became fixed when the pin was removed. ABAQUS could not find a solution when the forces were applied and the press-fit step was applied, since the press-fit was not resolved correctly. ABAQUS thought free body motion was occurring when it actually was not. I encountered this error when doing the convergence study. I increased the amount of memory allocated to the job, under the Edit Job tab, in order to solve this problem

6 Warning Degree of freedom 4,5,6 is not active in this model and can not be restrained The system matrix has 5 negative eigenvalues. Interpretation, Solution Degree of freedoms 4, 5, and 6 in ABAQUS refer to rotation about the x, y, and z axes respectively. A 3D solid element node cannot have rotation about these axes, since rotation is not supported in the node. These errors could be ignored because the boundary condition it was referring to, was also fixed in the x,y, and z directions translationally. It had no effect on the solution. To eliminate this warning, I could just get rid of the rotational boundary condition. This warning means that there is rigid body motion occurring. This is related to the error too many attempts made for this increment. This error was fixed when the press-fit pin was removed from the system No interaction property by specified name '"PRESS FIT"'. Contact pair definition will not written to the ODB. 40 nodes may have incorrect normal This warning meant that one of press-fit interactions either lever or drive shaft was not being used. This made it so that the press-fit did not fully resolve. One of the interactions would work properly, but the other would not. The ways I attempted to solve these issues is discussed below. This was due to the pin / lever interaction. To fix this problem I switched the master and the slave for the interaction, and the error was eliminated. definitions. 27 elements are distorted. This was due to the mesh quality not being within requirements at certain locations. As shown in Table 2, the mesh was good enough overall that this error could be ignored. These were the main errors and warnings that I encountered while running the file. The job could not complete if both the press-fit interaction and loads were applied. The system did not recognize both of the press-fits as being active, and therefore assumed that rigid body motion was occurring. To try and remedy this, I removed the applied loads, and just ran with the press fit. This led to nonphysical results shown in Figure 8. I then tried to change the master and slave surfaces for each interaction, but all led to nonphysical results. I tried creating separate steps for each of the press-fits, but this did not work either since automatic shrink fits can only be completed within the first step of the job. Knowing this, I made it so that one of the press-fits was not an automatic shrink fit, but rather a ramp to a uniform allowable interference of 0 inches. This did not work either. Figure 8. Initial results with just one press fit interaction working nonphysical results. The closest physical result that I obtained made it so that the drive shaft press fit worked properly, while the lever arm did not. I did this by making a tie constraint between the drive shaft and the lever arm, so that the action of Figure 8 did not occur. This resulting stress distribution is shown in Figure 9. The pin was the master surface for this interaction, with small sliding. Overlap can still be seen between the lever and the pin, since that step did not succeed

7 Figure 9. Resulting stress distribution due to the press fit pin (cut face). Only the drive shaft interaction is working properly, with a tie constraint between drive shaft and lever arm. As shown in Figure 9, the pin also slid in the assembly during the press-fit step. I added a boundary condition of no vertical displacement in order to counteract this. I tried putting this boundary condition in just the first 2 steps (not in the load step), since it would effect the loading, but it still slid down. I had to make this boundary condition active in all steps in order to prevent the sliding. This did not solve the problem of rigid body motion since the lever arm still did not possess any type of attachment to the pin. In order to get an estimate of the stresses from the model, I suppressed the pin from the model and tied the drive shaft to the lever arm. I then added boundary conditions of no motion on the internal faces where the pin would be. I did this in order to mimic the load sharing that would occur between the drive shaft and the lever arm, as well as the fact that no motion would occur at the press-fit. Post-Processing: Mesh Convergence: A mesh convergence was conducted for the model with no pin as described above. The area of interest for the lever arm was near the pin hole, so that is where I increased the number of elements. I used one of the partition, edge intersections to ensure that I took data from the same node. This model has a few stress concentrations in it so I needed to be careful of where I conducted the convergence study. There are also boundary conditions so I needed to make sure that I was far enough away from those so that it did not influence the results. Figure 10 shows the convergence of the model. This is done just for the lever arm since it is the area of interest. The majority of the drive shaft is controlled the by boundary conditions, so a convergence study did not prove useful

8 435 Von Mises Stress [psi] # Elements on Lever Arm Figure 10. Convergence study for overall model, varying elements on the lever arm. Comparison to Approximate Solutions: The pin did not work as expected within this model. I was unable to determine the stress in the lever arm due to the press fit, but was able to get an approximation of the stress in the drive shaft due to the press fit. As shown in Figure 9, the drive shaft experiences a max von Mises stress of ~91,000 psi. My hand calculations yielded a von Mises stress of approximately 43,000 psi, which is within an order of magnitude. Considering that I used pressure vessel equations, and the model did not completely run the press fit, this seems to be relatively close. My calculations also did not account for any concentration that may occur at the top of the shaft. Figure 11. Stress concentration at the pin, when no lever / drive shaft tie constraint or pin is used. My hand calculations for the lever arm did not assume load sharing from the drive shaft and pin. Running my model with the constraints mimicking my hand calculations I end up with the plot depicted in Figure 11. The max von Mises is roughly 2900 psi at the stress concentration, while my hand calcs predicted a stress about 1685 psi. These are within athe range of each other, - 8 -

9 and also it should be noted that as the mesh becomes finer, the FEA stress concentration continues to increase. FEA will naturally predict a stiffer structure, thus producing higher stresses. This is especially true due to the boundary condition at this point. Utilizing the tie constraint to mimic load sharing, with no pin, the deflection became what is shown in Figure 12. The von Mises stress in the lever was reduced to roughly 1062 psi, which is still close to the hand-calculated value. A max deflection in the vertical of.0027 inches is reported by ABAQUS, which is realistic for the small forces and scale of the model. Results: Figure 12. Deformed shape with stress distribution for tied constraint and no pin. Overall, the results were not as I anticipated. The press-fit did not work as intended and made the model as a whole more difficult to analyze. The results that I were able to get were in the range of my predicted values. The stress due to the press-fit was much higher than the stress due to the applied loads, which was as expected. Discussion: This project proved to be more difficult than was initially anticipated. The press-fit proved to be more challenging than was originally thought. If I were to do this again, I would probably not model the press-fit at all, but rather just the stresses due to the applied loads, since that is what I am interested in. I may just model the pieces as solids with a point constraint where the pin would be, so that the 2 pieces would stay aligned. Instead of a tie constraint, I would use a contact constraint between the two parts. This would lead to a more realistic view of the stress distribution within the part. I am not completely satisfied with the results and would like to reevaluate the model setup. This would make it so that the information I am interested in is accurate. This project did increase my knowledge of ABAQUS and its capabilities. I learned quite a bit about the step functionality, from defining steps, to incrementation, to the importance of step sequence. I also was able to experience importing parts from SolidWorks and creating 3D models. The meshing portion of the project was very challenging, due to some of the complex geometries. Creating partitions and varying the element sizes was useful in achieving a convergent mesh

10 Conclusions: The stress distribution due to the shrink fit could not accurately be found due to errors in ABAQUS. With the pin suppressed, and using tie constraints for the interaction between the lever and drive shaft (emulates load sharing), a von Mises stress of 1062 psi was obtained for the lever, which is close to the hand calculated value of 1685 psi. The overall deflection of the system was found to be.0027 inches. The press-fit interaction alone yielded a result of 91,000 psi between the pin and the drive shaft. This is in the ballpark of the hand calculated value of 43,300 psi for the lever. If this analysis were to be redone, then the press fit would need to work for both the lever and the drive shaft, or removed completely and replace with material or a boundary condition. This analysis yielded results that were in the expected range but needs to be re-evaluated for accuracy, since it needed to be greatly simplified in order to achieve results. References o o o o o Beer, Ferdinand et al. Mechanics of Materials. 3 rd Edition. Shigley, Joseph. Mechanical Engineering Design. 7 th Edition. Young, Warren. Roark s Formulas for Stress and Strain. 7 th Edition. ABAQUS Users Manual ABAQUS Theory Manual